PCB / fabrication print

Sounds like the "readme" text file that I send with my board orders.

Usually FR-4, 1/16" nominal thickness

Usually 1 ounce

I put the board outline (the actual shape of the finished board) on all layers as a .005" track

My usual "readme" files look something like this: ===============================

Job: 0929-3 Modular Motor Driver PC Board P-13162

The following files are required for this job: p13162.GTL Component side copper photoplot file p13162.GBL Solder side copper photoplot file p13162.GTO Component layout silkscreen p13162.GTS Top Solder Mask p13162.TXT Drill file readme.txt This file

Note: the Gerber files include embedded aperture data.

Drill Information Tool Hole Size Hole Count Plated Tool Travel

--------------------------------------------------------------------------- T1 28mil (0.7112mm) 57 45.83 Inch T2 35mil (0.889mm) 234 59.37 Inch T3 55mil (1.397mm) 10 12.06 Inch T4 63mil (1.6002mm) 15 15.61 Inch T5 110mil (2.794mm) 4 21.67 Inch T6 125mil (3.175mm) 8 14.71 Inch

--------------------------------------------------------------------------- Totals 328 169.25 Inch (4298.82 mm)

The board is approximately 8.8 x 3.94 inches, double-side, .0625" nominal thickness, FR-4 material

1 oz or greater copper Standard through-hole plating, standard tin-lead plating on exposed copper.

Solder mask both sides Component Ident silkscreen on component side

Trim boards to outline on component side artwork

Please make at least 20 boards.

=============================

--
Peter Bennett VE7CEI 
email: peterbb4 (at) interchange.ubc.ca        
GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html 
Newsgroup new user info: http://vancouver-webpages.com/nnq

All the data required is embedded in the various layers of the Layout file. This is translated into Gerber and Excellon by the CAM Processor.

If you haven't read David L. Jones' 25-page PDF yet, now would be a good time:

*-universities-*-*-*-*-*-are-*-including-it-as-*-reference-material-*-*-*-*-*-*-*-*-*+zz-zz+qq+*-major-*-PCB-*-package-*-*-included-it-in-their-Help-system

A previous thread related to this:

*-*-*-*-readme.txt-file-with-your-gerbers+zz-zz+qq+alignment+Fabrication-Information+Warp-*-twist+checklist

For general purpose work, you can use FR4. They don't actually use FR4 anymore, but the description will tell them to use the "standard" grade board material. 0.0625" (1.6mm) is a common thickness. Other less common board thicknesses are 0.031" and 0.093".

This is the thickness of the copper given in ounces/square foot. 1 ounce, or about 0.0012 to 0.0014", is common. For lots of small traces (smaller than 5 mil wide, 5 mil spacing) closely spaced, 0.5 ounce. For power circuitry, 1.5 to 4 oz.

This is the outline of your board edge. I put this info on the drill drawing. If the outline is complicated or I need the board put into a panel, I'll make a separate drawing with all useful dimensions in a 2D CAD program like AutoCad and include that drawing as a PDF. Of course, if you have a complicated board outline, I usually do the board outline in a 2D CAD program and export the board outline to the PCB layout program.

Some boards have material removed from the center portion. This can be shown in the drawing showing board outline

You need to tell the board house the order of the layers, what material to use, copper thickness, buried and blind via layer associations, board material type, and anything else that is pertinent.

You should be able to put all information about your board using Eagle. If you need to supply an additional 2D drawing, use any 2D drafting package and include that drawing as a PDF.

It is customary to only have an even number of layers as this reduces manufacturing costs for the board house. If you have an odd number of layers, think about duplicating a ground layer to make it even.

A simple board submission will include the following files:

1. Gerber files (files with trace and pad info for each layer)
2. Excellon drill file(s) (drill hole file)
3. Readme file with your contact info, descriptions of each file in your submission to the board house, board details (copper thickness, board thickness, board material, layer order, number of layers, number of drill holes, number of different hole sizes, special instructions, etc).

Pack everything up in a ZIP file.

You may find this web site of interest:

--
Mark